/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2011-2025 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Class
    Foam::contactAngleFvPatchScalarField

Description
    General alpha contact angle boundary condition.

    The essential entry "limit" controls the gradient of alpha1 on the wall:
      - none - Calculate the gradient from the contact-angle without limiter
      - gradient - Limit the wall-gradient such that alpha1 remains bounded
        on the wall
      - alpha - Bound the calculated alpha1 on the wall
      - zeroGradient - Set the gradient of alpha1 to 0 on the wall, i.e.
        reproduce previous behaviour, the pressure BCs can be left as before.

    Note that if any of the first three options are used the boundary condition
    on \c p_rgh must set to guarantee that the flux is corrected to be zero at
    the wall.

Usage
    \table
        Property     | Description                  | Required | Default value
        limit        | Limiting option              | yes      |
        contantAngle | Contact angle model settings | no       | none
    \endtable

    Example of the boundary condition specification for a constant angle:
    \verbatim
    <patchName>
    {
        type            contactAngle;
        limit           none;
        contactAngle
        {
            type            constant;
            theta0          70;
        }
    }
    \endverbatim

    If the contactAngle sub-dictionary is not given, a constant angle will be
    assumed. Example:
    \verbatim
    <patchName>
    {
        type            contactAngle;
        limit           none;
        theta0          70;
    }
    \endverbatim

See also
    Foam::contactAngleModel
    Foam::contactAngleModels::constant
    Foam::contactAngleModels::dynamic

SourceFiles
    contactAngleFvPatchScalarField.C

\*---------------------------------------------------------------------------*/

#ifndef contactAngleFvPatchScalarField_H
#define contactAngleFvPatchScalarField_H

#include "fixedGradientFvPatchFields.H"
#include "contactAngleModel.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam
{

/*---------------------------------------------------------------------------*\
             Class contactAngleFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/

class contactAngleFvPatchScalarField
:
    public fixedGradientFvPatchScalarField
{
public:

    // Public Enumerations

        //- Alpha limit options
        enum limitControls
        {
            lcNone,
            lcGradient,
            lcZeroGradient,
            lcAlpha
        };

        //- Alpha limit option names
        static const NamedEnum<limitControls, 4> limitControlNames_;


private:

    // Private Data

        //- Equilibrium contact angle function
        autoPtr<contactAngleModel> contactAngle_;

        //- Alpha limiting option
        limitControls limit_;


public:

    //- Runtime type information
    TypeName("contactAngle");


    // Constructors

        //- Construct from patch, internal field and dictionary
        contactAngleFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );

        //- Construct by mapping given contactAngleFvPatchScalarField
        //  onto a new patch
        contactAngleFvPatchScalarField
        (
            const contactAngleFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fieldMapper&
        );

        //- Disallow copy without setting internal field reference
        contactAngleFvPatchScalarField
        (
            const contactAngleFvPatchScalarField&
        ) = delete;

        //- Copy constructor setting internal field reference
        contactAngleFvPatchScalarField
        (
            const contactAngleFvPatchScalarField&,
            const DimensionedField<scalar, volMesh>&
        );


    // Member Functions

        //- Return the cosine of the contact angle
        tmp<scalarField> cosTheta
        (
            const fvPatchVectorField& Up,
            const vectorField& nHat
        ) const;

        //- Evaluate the patch field
        virtual void evaluate
        (
            const Pstream::commsTypes commsType=Pstream::commsTypes::blocking
        );

        //- Write
        virtual void write(Ostream&) const;


    // Member Operators

        //- Inherit assignment
        using fixedGradientFvPatchScalarField::operator=;
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

} // End namespace Foam

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

// ************************************************************************* //
